[cmoreno98]

Hello everybody,

I'm running some simulations in a T-junction (water enters through the vertical pipe and air through the horizontal one) using interFoam. The full case folder can be downloaded HERE (includes a .log file of the last simulation).

The geometry and the mesh are the following (428k cells):






Something strange is happening at the outlet, bubbles are not leaving the pipe in a proper way. These are the last pictures of the simulation, before the Courant number blows up:




Air velocity is 0.5 m/s, water velocity is also 0.5 m/s. DeltaT is 1e-6, endTime is 0.0512. I paste here alpha.air, p_rgh and U files:

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  6
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      alpha.air;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 0 0 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    inlet1
    {
        type            fixedValue;
        value           uniform 1;
    }

    inlet2
    {
        type            fixedValue;
        value		uniform 0;
    }

    walls1
    {
        type            constantAlphaContactAngle;
        theta0          155;
        limit           gradient;
        value           uniform 0;
    }

    walls2
    {
        type            fixedValue;
        value		uniform 0;
    }

    outlet
    {
        type            zeroGradient;
    }
}

// ************************************************************************* //

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  6
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [1 -1 -2 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    inlet1
    {
        type            fixedFluxPressure;
        value           $internalField;
    }

    inlet2
    {
        type            fixedFluxPressure;
        value           $internalField;
    }

    walls1
    {
        type            zeroGradient;
    }

    walls2
    {
        type            zeroGradient;
    }

    outlet
    {
        type            fixedValue;
	value		$internalField;
    }
}

// ************************************************************************* //

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  6
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    location    "0";
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
    inlet1
    {
        type            fixedValue;
        value           uniform (0.5 0 0);
    }

    inlet2
    {
        type            fixedValue;
        value           uniform (0 -0.5 0);
    }

    walls1
    {
        type            noSlip;
    }

    walls2
    {
        type            noSlip;
    }

    outlet
    {
        type            zeroGradient;
    }
}

// ************************************************************************* //

I don't know where the error is. Outlet BC are zeroGradient for alpha.air and U files and fixedValue uniform 0 for pressure file (atmospheric pressure), all of them make sense to me.

What should I change? Any help is appreciated,

Carlos

[cmoreno98]

Can someone help me, please?

[cmoreno98]

I would appreciate it

[gkarlsen]

Hi,

I downloaded and modified your case as follows:
Controldict:
AdjustTimeStep: Yes
MaxCo: 1
MaxAlphaCo: 0.5

Boundary conditions for outlet patch:
U: pressureInletOutletVelocity
p_rgh: prghTotalPressure, P0 uniform 1e5
alpha.air: inletOutlet, inletvalue 0

Seems to run just fine. The time step is low, but that is to be expected as your geometry is only about 6 mm long. The velocity is quite significant for such a small geometry

Animation of my results:
https://drive.google.com/file/d/19v-...ew?usp=sharing

[cmoreno98]

Originally Posted by gkarlsen

Hi,

I downloaded and modified your case as follows:
Controldict:
AdjustTimeStep: Yes
MaxCo: 1
MaxAlphaCo: 0.5

Boundary conditions for outlet patch:
U: pressureInletOutletVelocity
p_rgh: prghTotalPressure, P0 uniform 1e5
alpha.air: inletOutlet, inletvalue 0

Seems to run just fine. The time step is low, but that is to be expected as your geometry is only about 6 mm long. The velocity is quite significant for such a small geometry

Animation of my results:
https://drive.google.com/file/d/19v-...ew?usp=sharing

Hello gkarlsen,

thank you very much! The key was to activate AdjustTimeStep, limiting the Courant number. I have 2 questions:

1. How do you export the results of the simulation in 3D? (the .avi file that you have shared)
2. If you have a look at the outlet, the diameter of the bubbles gets smaller when leaving the geometry. Is there a way to modify it? It looks like they are being "absorbed" at the exit. Which boundary condition should we change? I want the bubbles to remain the same size when they go through the outlet.

Thank you in advance,

Carlos

[gkarlsen]

Originally Posted by cmoreno98

Hello gkarlsen,

1. How do you export the results of the simulation in 3D? (the .avi file that you have shared)
2. If you have a look at the outlet, the diameter of the bubbles gets smaller when leaving the geometry. Is there a way to modify it? It looks like they are being "absorbed" at the exit. Which boundary condition should we change? I want the bubbles to remain the same size when they go through the outlet.

Hi, glad you got it to work

I used paraview "save animation" to export each timestep to a png. You can combine these to make a video file. The filter used is "clip" set to alpha scalar (not inverted). Reduce opacity to "see through" the bubbles.

It could be advantageous to extend your computational domain if you want to capture the actual flow conditions at the outlet. Are you trying to replicate experimental conditions? Is your geometry actually submerged in water or air?

[cmoreno98]

Originally Posted by gkarlsen

Hi, glad you got it to work

I used paraview "save animation" to export each timestep to a png. You can combine these to make a video file. The filter used is "clip" set to alpha scalar (not inverted). Reduce opacity to "see through" the bubbles.

Thanks, I'll do it the next time.

Originally Posted by gkarlsen

It could be advantageous to extend your computational domain if you want to capture the actual flow conditions at the outlet. Are you trying to replicate experimental conditions? Is your geometry actually submerged in water or air?

Yes, I want to replicate an experiment. The following picture shows the experiment results (left) and the results of a simulation that Aboukhedr et al. (2018 paper) did in OpenFOAM (right):



Here the inlets are changed (liquid through the horizontal and air through the vertical), but the results at the outlet should be similar.
In both cases the bubbles are exiting the geometry without any deformation. I want to replicate this behavior. I don't know if just changing some BC I can get this result or if the problem is more complex.


In the paper they use the following BCs:



I copied the BCs and I got the same results as before, the diameter of the bubbles gets smaller at the outlet... Any idea?

Thank you very much gkarlsen

[gkarlsen]

There is probably a "correct" way to do this, but personally I would just elongate the horizontal part of the pipe for the simulation, and then cut it back to size during post processing. This should eliminate the disturbance from the BC at the outlet. I do not think bubbles would exit undisturbed in real life. The bouyancy/gravity alone could warp them.

[mumuaye]

Hello

I'm new to OpenFOAM and I'm trying to run a similar question. The blockMesh has always been unsuccessful, can you give me a blockMesh file?

Thank you.